Mirror Body & Hide Original

[ingallspw]

I am using NX 7.5.
Is there a way to automatically hide (not suppress) the body you are mirroring?
See "Instance Geometry" >> "Hide Original" as an example.

(We have complicated parts that are merely mirrors of each other. I have the mirror body command setup to unsuppress using expressions but the original still shows and it can be confusing to other users which is which.)

 

[ChaseWichert]

What about if you used body colors? Make all of the mirrored components a certain color therefore you knew which one was which. When I suppress and unsuppress the instance geometry feature it keeps the body color that I set. I am not sure if there is an easy way to hide the original bodies.

NX 8.5.1.3

 

[zanouk]

Hello ingallspw,

I don't know of any way of automatically hiding a body you want to mirror, but in my opinion the best way to obtain what you want is to move the object you plan to mirror on a different layer and then just hide the layer on which the original object is.

I work with layers for bodies when different manufacturing procedures are done on one part and we need to show the steps on only one drawing. I have a hotkey assigned for joggling with layers from the space mouse so it's all very fast and efficient. Just select and deselect.

Hope this helps in any way.

 

[ingallspw]

Can i revive the dead here for a moment... I am not sure if I explained what I really wanted very well.

All I want to do is have an exact replica of my current part but mirrored without the original part sticking around. I attached a Q&D example pic. I want to keep the yellow and "delete" the red x part. (I don't want to simply hide it, pretend like it doesn't exist, nor do I want to have a unpasteurized dummy file if that makes since.)

At minimum, can someone explain why you can't do this? We are running into problems all over leaving it with two bodies. Export has a major issue with it unless you use select bodies but not everyone remembers which models need you to export like this.

Thanks ju all!

I'm using NX7.5 still. We are moving to NX9 first quarter next year.

 

[JohnRBaker]

Your original post was asking for some way to 'Hide' the parent body, but now you seem to be asking about how to get rid of it altogether. Is that true?

For NX 7.5 you don't have any easy solutions if that's what you really want to do, get rid of the parent. The best that you do now is remove the parametrics (make the model 'dumb') by going to...

Edit -> Feature -> Remove Parametrics...

...and selecting the Mirrored Body. Once you've done that, you can then delete the 'parent' body. Of course this means that there will be no way to reconnect your model back to it's parent.

Now there is one thing that you could do and that would be to create the Mirrored Body as part of WAVE linking operation where the new Mirrored Body is in a separate part file. This way, there is ONLY a WAVE link to the 'parent' part file. This means that when you export the Mirrored Body it will only see what's in that part file and will ignore the WAVE link since that body in in another part file altogther.

Note that starting with NX 8.5 we have added a function which will do exactly what you're looking without having to either 'REmove Parametrics' or create a WAVE linked part file. In NX 8.5 we added a new function that will allow you to 'Delete' a body in such a way that as far as any downstream operation is concerned, such as exporting the model to IGES or STEP or whatever, that it will never see the 'parent' body even though the Mirrored Body is still a feature and is still a 'child' of the original, now 'deleted' parent. Note that this is NOT the same as a simple 'Edit -> Delete...' operation since that will remove the 'child' as well as the 'parent'. No, the new 'Delete Body' operation removes the body from the part file but does NOT remove it from the history of the Mirrored Body. And one other thing, you can come back any time that you wish and remove this 'Delete Boy' operation and restore the 'parent' so that it can be edited so that the 'child', the Mirrored body, will now update to reflect those changes made to its 'parent'.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[ingallspw]

I think when I first wrote this I had read what I am asking now was impossible so I submitted to hide the body. But its just becoming a hassle now.

I really don't want to delete it...

Ahh ok... its like this:

Lets say I am using Edit > Move Body, select "Move Original" and have "Associative" checked. The body moves, creates a Move Object in the part navigator, but it does not create a copy to move it, leaving the original. The original simply moved.

I want to do the same thing with mirror body. No duplicate part but all the history.

(Maybe if I threw it in a scenario... What if I spent 8 weeks developing a part and a bigshot with a master's degree comes down and says, "I Changed my mind... I want this to be mirrored." No biggy... but it is a big deal in a way, because now the model has two bodies and not just the one...)

Thank you kind sir for your reply!

 

[JohnRBaker]

OK, that's exactly what that new NX 8.5 'Delete Body' function will accomplish.

In the case of the 'Move Body', NX is doing just that, it's MOVING the body, period. In the case of the Mirror Body, it's NOT flipping the original one inside-out as it were, but rather creating a Mirrored 'child'. The concepts are NOT equivalent, as one case, the Move, does not create a parent->child relationship while the other one does. And in order to have a parent->child relationship you have to have TWO bodies. That just the way it works, which of course was part of what motivated us to add the NX 8.5 'Delete Body' function in the first place, so that NX could retain a parent->child relationships WITHOUT having to keep TWO bodies in the part file. Sort of like "NOT having your cake, but still being able to eat it" ;-)

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[KhimaniMohiki]

You also need to ensure 'Fix at current Timestamp' is turend on

Khimani Mohiki
Design Engineer - Aston Martin
NX8.5

 

[ingallspw]

Oh I get it now!

Yeah!!!! I like cake! I look forward to the upgrade (I hope soon)!!!

Thanks man!